Help slotting ar400

I had a little job today where I needed to slot some ar400 plate. It is basically a rectangular plate with 27 slots 3/8" wide by 2 1/2" long. It resembles a floor drain plate but I'm sure that is not what its for. The plate is 3/4" thick and the slots go all the way through. I thought the endmill would have trouble plunging this ar400 so I drilled the end of all the slots. Then I tried to mill the slots with a 5/16 carbide endmill and then I was going to finish with a 3/8" endmill. I tried a .100" depth of cut at 12 in/min and 3000 rpms. That quickly broke a cutter. Then I tried .075" depth of cut and slower feed. Still broke a cutter after about 2 slots. I had the best luck with 1400 rpm and 3 in/min feed. I still can only get about 3 slots before the cutter breaks. I gave up and need help. Lol What seems to be the problem is that the edges of the holes that I drilled are work hardened. I plunge into the drilled hole and it makes noise when it starts to mill longitudinally until it gets through the hardened edge of the hole. I drilled the holes with a 11/32 high speed drill but for some reason it work hardened the edges of the hole. By the time I get one slot milled out the last .100 of the endmill is about toast. Any help would be appreciated. We might end up getting the slots water jetted.

water jet would be the way to go without a doubt. if you had to cut it with a endmill I'd be more conservative like .05 dept and 1 inch a min and 900 to 1000 rpm. I'd also consider doing volume mill type pass where you are side cutting about. 02 a pass with increased depth like .1, as well as feed and speed.

I forgot I also tried to plunge mill a few slots. I stepped over .100 for each plunge and ran 2.5 in/min feed and 1400 rpm but this also only produced about 3 slots before the cutter gave up the ghost.

If you want to avoid having to waterjet, then try using a good, sharp carbide drill to drill a new start hole just inside one of the previous end holes (just one end), then use a 1/4 x 1/2 stub endmill to troicoidal the rough slot width at 1/2 depth. Watch the cut, if the endmill shows excessive signs of wear swap to a fresh one.

Slow feed/speed when you get to the previous drilled areas to lessen the damage against the WH surfaces. Use a quality AlTiN or similar coated tool, and check with the manufacturer about whether to use an air blast rather than coolant.

When you get one side done, flip and finish the second side through. For finishing, I'd want to use an undersize endmill at full depth so that you're not rubbing on the "conventional" side, and maybe use a six flute tool meant for die finishing so you can get a rigid core. Anyone make a 9mm six fluter?

Did you check the condition of the HSS drill you used for the pilot holes? Did one drill do them all?

I sharpened the drill before I started and it drilled all the holes without sharpening. Whats weird is the first hole was just as worked hardened as the last one. I actually plunged a 3/8 carbide endmill in all the holes to try and get rid of the hard edge but the hard edge extends out past the reach of the 3/8 endmill. I could step over .100 on all the holes and plunge mill to get rid of the hard edge and then try to mill the slots after that. I could flip it over after going going half way through but it would be hard to get set up since the plate is only burned out on the outside edges. I could indicate one of the holes though and keep the same side against the solid jaw of the vise.

I had a little job today where I needed to slot some ar400 plate. It is basically a rectangular plate with 27 slots 3/8" wide by 2 1/2" long. It resembles a floor drain plate but I'm sure that is not what its for. The plate is 3/4" thick and the slots go all the way through. I thought the endmill would have trouble plunging this ar400 so I drilled the end of all the slots. Then I tried to mill the slots with a 5/16 carbide endmill and then I was going to finish with a 3/8" endmill. I tried a .100" depth of cut at 12 in/min and 3000 rpms. That quickly broke a cutter. Then I tried .075" depth of cut and slower feed. Still broke a cutter after about 2 slots. I had the best luck with 1400 rpm and 3 in/min feed. I still can only get about 3 slots before the cutter breaks. I gave up and need help. Lol What seems to be the problem is that the edges of the holes that I drilled are work hardened. I plunge into the drilled hole and it makes noise when it starts to mill longitudinally until it gets through the hardened edge of the hole. I drilled the holes with a 11/32 high speed drill but for some reason it work hardened the edges of the hole. By the time I get one slot milled out the last .100 of the endmill is about toast. Any help would be appreciated. We might end up getting the slots water jetted.

In the Green part you are running 225 SFM, then you slowed down to 1400 RPM which is still 114 SFM. I would run around 45 SFM with a carbide Endmill....so 550 RPM with a .3125" Endmill, similar chipload though, so the change would be about 2 IPM at 550 RPM. AR400 is a nightmare to work with. If you can generate the holes you're doing okay, but Drills are tough tools, Endmills aren't.

I often work with AR500 and 46100E (hence the name hardplates). Troicoidal, adaptive, profit milling, high speed machining or whatever you want to call it is your friend here. I am rather conservative with my radial engagement and would start around .005-.010" and take the depth in 2 separate wacks. But I would run 300-500 fpm and start around a .001" per tooth feed. 400 is a good bit softer than 500, no fancy endmills needed, just quality carbide works for me. Also if your predrilled hole are still giving you trouble you can take 1 pass around them conventional milling to help get under the work hardening.

Take a look at some hardmilling speeds and feeds online. This isn't what "I" would call hardmilling but it can help to show you what direction to head it with speeds and feeds.

I often work with AR500 and 46100E (hence the name hardplates). Troicoidal, adaptive, profit milling, high speed machining or whatever you want to call it is your friend here. I am rather conservative with my radial engagement and would start around .005-.010" and take the depth in 2 separate wacks. But I would run 300-500 fpm and start around a .001" per tooth feed. 400 is a good bit softer than 500, no fancy endmills needed, just quality carbide works for me. Also if your predrilled hole are still giving you trouble you can take 1 pass around them conventional milling to help get under the work hardening.

Take a look at some hardmilling speeds and feeds online. This isn't what "I" would call hardmilling but it can help to show you what direction to head it with speeds and feeds.

I don't know about waterjet but on my plasma table I would charge $0.20 a pierce and $0.15 an inch. Waterjets have a higher operating cost and are much much slower so maybe that might help you guess pricing....

What are you machining these on? Try something similar to garr vrx , 9/32 x 7/16 LOC to rough with. Machine slot using a trochoidal type path in 2 passes at about .4 doc, offset second pass about .01 from first to avoid shanking out. Finish slot with 9/32 or 5/16 x 13/16 loc.

Im running this on a mazak vtc 16. Unfortunately i have no way to generate code for a trochoidal tool path.

No CAM? Time to download and try out Fusion...

Can you draw in CAD? Try a repeated "C" shape, with the curve of the C in the direction of travel, and spaced about .007-.010 one to the next. Then map out coordinates with whatever offset needed for the tool diameter you're using.

Can you draw in CAD? Try a repeated "C" shape, with the curve of the C in the direction of travel, and spaced about .007-.010 one to the next. Then map out coordinates with whatever offset needed for the tool diameter you're using.

I was thinking the exact same thing! A small straight slot shouldn't be to difficult to hand write trochoidal(ish) G-code, a pain yes but can definitely be done. Probably quicker and easier to just try Fusion though.

Are you getting the chips evacuated and out of the way? Cutting dry with air blast is preferred. I would straight slot it with the 3/8 end mill. Depth of cut will be limited, as the slot depth is twice the cutter diameter. 90% of my work is 400-500 wear steels. 400 should machine well at 300+SFM. Make sure you are not pausing in the cut anywhere, especially if you are manually programming. Is this a quality brand name tool, or some MSC garbage?

I am going out on a limb here but a good solid carbide roughing corncob style endmill with moderate helix with enough cut length is what I would use for roughing. Many companies make them Niagara SR420 style are pretty good.

Drop in your predrilled hole and cut adjust your feed to not just break off the endmill cutting full depth.

An advantage of going all the way through on the first cut is a place for the chips to go.

Posting Permissions

ABOUT Practical Machinist

With more than 10.6 million unique visitors over the last year, Practical Machinist is the most visited site for metalworking professionals. Practical Machinist is the easiest way to learn new techniques, get answers quickly and discuss common challenges with your peers. Register for the world’s largest manufacturing technology forum for free today to stay in the know.

This website or its third-party tools use cookies, which are necessary to its functioning and required to achieve the purposes illustrated in the cookie policy. If you want to know more or withdraw your consent to all or some of the cookies, please refer to the cookie policy.

By closing this banner, scrolling this page, clicking a link or continuing to browse otherwise, you agree to the use of cookies.

The latest industry news—straight to your inbox

Sign up for our eNewsletter now to stay in-the-know. We'll bring you the most relevant peer-to-peer conversations happening in the trade and tips and tricks to help you get the job done.

Name:

Email:

Invalid email

I agree to receive emails from Practical Machinist containing industry news and updates from Practical Machinist and its sponsors. You may unsubscribe at any time.